2.5D MILLING Training Course InventorCAM+Inventor The complete integrated Manufacturing Solution Autodesk® Inventor® 2013 Certied
InventorCAM 2013 Milling Training Course 2.5D Milling ©1995-2012 SolidCAM All Rights Reserved.
Contents v Contents 1. Introduction 1.1 About this course............................................................................................................................3 1.2 Basic Concepts................................................................................................................................5 1.3 Process Overview...........................................................................................................................5 2. CAM-Part Definition Exercise #1: CAM-Part Definition.............................................................................................9 3. InventorCAM 2.5D Operations Exercise #2: Cover Machining ..................................................................................................30 Exercise #3: Cover Machining ..................................................................................................84 Exercise #4: Bracket Machining .............................................................................................153 Exercise #5: Electronic Box Machining ................................................................................155 Exercise #6: Clamp Machining ...............................................................................................158 Exercise #7: Basic Part Machining .........................................................................................166 Exercise #8: Cover Machining ................................................................................................170 Exercise #9: Mounting Base Machining................................................................................177 Exercise #10: Support Machining ..........................................................................................187 4. Indexial 4-Axis Milling Exercise #11: Frame Machining .............................................................................................199 Exercise #12: Mounting Machining .......................................................................................220 5. Indexial 5-Axis Milling Exercise #13: Clamp Machining.............................................................................................231
vi 6. ToolBox Exercise #14: Standard Cycles Machining.............................................................................240 7. Automatic Feature Recognition Exercise #15: Pocket Recognition..........................................................................................255 Exercise #16: Mounting Box Machining...............................................................................262 Exercise #17: Drill Recognition..............................................................................................264 Exercise #18: Electronic Box Machining ..............................................................................289 Document number: ICMTCENG12001
Introduction 1
2
3 1. Introduction 1.1 About this course The goal of this course is to teach you how to use InventorCAM to machine various parts using 2.5D Milling technologies. This course covers the basic concepts of InventorCAM 2.5D machining and is a supplement to the system documentation and online help. Once you have developed a good foundation in basic skills, you can refer to the online help for information on the less frequently used options. Course design This course is designed around a task-based approach to training. With the guided exercises you will learn the commands and options necessary to complete a machining task. The theoretical explanations are embedded into these exercises to give an overview of the InventorCAM 2.5D Milling capabilities. Using this training book This training book is intended to be used both in a classroom environment under the guidance of an experienced instructor and as self-study material. It contains a number of laboratory exercises to enable you to apply and practice the material covered by the guided exercises. The laboratory exercises do not contain step-by-step instructions. About the CD The CD supplied together with this book contains copies of various files that are used throughout this course. The Exercises folder contains the files that are required for guided and laboratory exercises. The Built Parts folder inside the Exercises contains the final manufacturing projects for each exercise. Copy the complete Exercises folder on your computer. The Autodesk Inventor files used for the exercises were prepared with Autodesk Inventor 2013. Windows 7 The screenshots in this book were made using InventorCAM 2013 integrated with Autodesk Inventor 2013 running on Windows 7. If you are running on a different version of Windows, you may notice differences in the appearance of menus and windows. These differences do not affect the performance of the software.
4 Conventions used in this book This book uses the following typographic conventions: Bold Sans Serif This style is used to emphasize InventorCAM options, commands or basic concepts. For example, click the Change to opposite button. 10. Define CoordSys Position The mouse icon and numbered sans serif bold text indicate the beginning of the exercise action. Explanation This style combined with the lamp icon is used for the InventorCAM functionality explanations embedded into the guided exercises. The lamp icon is also used to emphasize notes.
5 1. Introduction 1.2 Basic Concepts Every manufacturing project in InventorCAM contains the following data: • CAM-Part – The CAM-Part defines the general data of the workpiece. This includes the model name, the coordinate system position, tool options, CNC-controller, etc. • Geometry – By selecting Edges, Curves, Surfaces or Solids, define what and where you are going to machine. This geometry is associated with the native Autodesk Inventor model. • Operation – An Operation is a single machining step in InventorCAM. Technology, Tool parameters and Strategies are defined in the Operation. In short, Operation means how you want to machine. 1.3 Process Overview The major stages of the InventorCAM manufacturing project creation process are the following: CAM-Part definition This stage includes the definition of the global parameters of the Manufacturing Project (CAM-Part). You have to define a number of Coordinate Systems that describe the positioning of the part on the CNC-machine. Optionally, you can define the Stock model and the Target model to be used for the rest material calculation. The Stock model describes the initial state of the workpiece that has to be machined. The Target model describes the one that has to be reached after the machining. After every operation, InventorCAM calculates how much material was actually removed from the CAM-Part and how much material remains unmachined (rest material). The rest material information enables InventorCAM to automatically optimize the tool path and avoid the air cutting. Operations definition InventorCAM enables you to define a number of milling operations. During an operation definition you have to select the Geometry, choose the tool from the Part Tool Table (or define a new one), define a machining strategy and a number of technological parameters.
6
CAM-Part Definition 2
8 The CAM-Part definition process includes the following stages: • CAM-Part creation. At this stage, you have to define the CAM-Part name and location. InventorCAM defines the necessary system files and a folder to allocate the place to store InventorCAM data. • CNC-controller definition. Choosing a CNC-controller is a necessary step. The controller type influences the Coordinate System definition and the Geometry definition. • Coordinate System definition. You have to define the Coordinate System – the origin for all machining operations of the CAM-Part. • Stock model definition. InventorCAM enables you to define the stock model that describes the initial state of the workpiece that has to be machined. • Target model definition. InventorCAM enables you to define the model of the part in its final state after the machining. CAM-Part creation Coordinate System definition Stock model definition CNC-controller definition Target model definition
9 2. CAM-Part Definition Exercise #1: CAM-Part Definition This exercise illustrates the process of the CAM-Part definition in InventorCAM. In this exercise, you have to create the CAM-Part for the cover model displayed and define the Coordinate System, the Stock model and the Target model that are necessary for the part machining. The CAM-Part will be used in the exercises further on. When you start to program a CAM-Part, you have to decide what workpiece you are going to use. This decision determines the number and the type of operations that are used to reach the final part shape. In this exercise, the box stock is used. The box dimensions include offsets from the actual model. At the next stage, you have to decide on what type of CNC-machine you are going to use (3-, 4- or 5-axis). In this exercise, a 3-axis CNC-machine is chosen for the machining. With a CNC-machine of this type, all the required faces of the cover part can be machined using a single positioning.
10 1. Load the Autodesk Inventor model Load the Exercise1.ipt model located in the Exercises folder. This model contains a number of features forming the solid body of the cover. 2. Start InventorCAM To activate InventorCAM, click the InventorCAM 2013 field in the main menu of Autodesk Inventor and choose Milling from the New submenu. InventorCAM is started and the New Milling Part dialog box is displayed.
11 2. CAM-Part Definition New Milling Part dialog box When you create a new CAM-Part, you have to enter a name for the CAM-Part and for the model that contains the CAM-Part geometry. Directory Specify the location of the CAM-Part. The default directory is the InventorCAM user directory (defined in the InventorCAM Settings). You can enter the path or use the Browse button to define the location. The Use Model file directory option enables you to automatically create CAM-Parts in the same folder where the original CAD model is located. CAM-Part name Enter a name for the CAM-Part. You can give any name to identify your machining project. By default, InventorCAM uses the name of the design model. Model name This field shows the name and location of the Autodesk Inventor design model that you are using for the CAM-Part definition. The name is, by default, the name of the active Autodesk Inventor document. With the Browse button you can choose any other Autodesk Inventor document to define the CAM-Part. In this case, the chosen Autodesk Inventor document is loaded into Autodesk Inventor. Every time the CAM-Part is opened, InventorCAM automatically checks the correspondence of the dates of the CAM-Part and the original Autodesk Inventor design model. When the date of the original Autodesk Inventor model is later than the date of the CAM-Part creation, this means that the Autodesk Inventor original model has been updated. You can then replace the Autodesk Inventor design model on which the CAM-Part is based with the updated Autodesk Inventor design model.
12 3. Confirm the CAM-Part creation When the Directory, CAM-Part name and Model name have been defined, click the OK button to confirm the CAM-Part creation. The CAM-Part is defined and its structure is created. The Milling Part Data dialog box is displayed. 4. Choose the CNC-Controller Select the CNC-machine controller. Click the arrow in the CNC-Machine area to display the list of post-processors installed on your system. In this exercise, use a 3-axis CNC-machine with the AWEA1000-Fanuc CNC-controller. Choose the AWEA1000-Fanuc CNC-controller from the list. 5. Start the Coordinate System definition Click the Define button in the CoordSys area to define the Machine Coordinate System. To complete the CAM-Part definition, you need to define the Machine Coordinate System. The Machine Coordinate System defines the origin for all machining operations of the CAM-Part. It corresponds with the built-in controller functions.
13 2. CAM-Part Definition You can define the Coordinate System origin position and axes orientation by selecting model faces, vertices, edges or Inventor Coordinate Systems. The geometry for the machining can also be defined directly on the solid model. The Z-direction of the Machine Coordinate System is parallel to the revolution axis of the tool. In InventorCAM, the tool approaches from the positive direction of the Z-axis (like on a vertical CNC-machine). For 3-axis CNC milling machines, each Machine Coordinate System means separate clamping. If you need to machine the part from different sides, use several Machine Coordinate Systems with the Z-axis oriented normally to the machined sides. X Z Y Machine Coordinate System X Z Y Coordinate System X Z Y X Z Y Coordinate System Coordinate System
14 In this exercise, it is enough to define one Machine Coordinate System with the Z-axis oriented upwards. Such coordinate system enables you to machine the part with a single clamping. The CoordSys dialog box enables you to define the Coordinate System location and the orientation of the axes. InventorCAM enables you to define the CoordSys using the following methods: Select Face This method enables you to define a new CoordSys by selecting a face. The face can be either planar or cylindrical/conical. For planar faces, InventorCAM defines CoordSys with the Z-axis normal to the face. For cylindrical or conical faces, the Z-axis of the CoordSys is coincident with the axis of revolution of the specified cylindrical/ conical surface. X Z Y Coordinate System
15 2. CAM-Part Definition Define This method enables you to define the Coordinate System by selecting points. You have to define the origin and the direction of the X- and the Y-axes. Select Coordinate System This method enables you to choose the Autodesk Inventor Coordinate System defined in the design model file as the CoordSys. The CoordSys origin and axes orientation are the same as those of the original Autodesk Inventor Coordinate System. Normal to current view This option enables you to define the Coordinate System with the Z-axis normal to the model view you are facing on your screen. The CoordSys origin will lie in the origin of the Autodesk Inventor Coordinate System, and the Z-axis will be directed normally to the chosen view of the model. By 3 Points (Associative) This option enables you to define the Coordinate System by selecting any 3 points. 6. Select the model face With the Select Face method chosen, click the model face as shown. The CoordSys origin is automatically defined in the corner of the model box. The Z-axis of the CoordSys is normal to the selected face.
16 Coordinate System X Z Y Model box InventorCAM calculates the box surrounding the model. The upper plane of the model box is parallel to the XY-plane of the defined CoordSys. The CoordSys is located in the corner of the model box. Confirm by clicking the Finish button. The Coordinate System is defined. The CoordSys Data dialog box is displayed. 7. CoordSys Data This dialog box enables you to define the Machining levels such as Tool start level, Clearance level, Part upper level, etc.
17 2. CAM-Part Definition CoordSys Data dialog box The Position field defines the sequential number of the CoordSys. For each Machine Coordinate System, several Position values are defined for different positions; each such Position value is related to the Machine CoordSys. • X shows the X value of the CoordSys. • Y shows the Y value of the CoordSys. • Z shows the Z value of the CoordSys. The Machine CoordSys number defines the number of the CoordSys in the CNC-machine. The default value is 1. If you use another number, the GCode file contains the G-function that prompts the machine to use the specified number stored in the machine controller of your machine. The Tool start level defines the Z-level at which the tool starts working. The Clearance level is the Z-level to which the tool moves rapidly from one operation to another (in case the tool does not change). The Part upper level defines the height of the upper surface of the part to be milled. The Part lower level defines the lower surface level of the part to be milled. The Tool Z-Level parameter defines the height to which the tool moves before the rotation of the 4/5 axes to avoid collision between the tool and the workpiece. This level is related to the CoordSys position and you have to check if it is not over the limit switch of the machine. Rapid movements area Feed movements area Part Upper level Part Lower level Tool start level Clearance level
18 It is highly recommended to send the tool to the reference point or to a point related to the reference point. The Create planar surface at Part Lower level option enables you to generate a transparent planar surface at the minimal Z-level of the part so that its lower level plane is visible. This planar surface provides you the possibility to select points that do not lie on the model entities. It is suppressed by default and not visible until you unsuppress it in the Model elements tree. Confirm the CoordSys Data dialog box with the OK button. The CoordSys Manager dialog box is displayed. This dialog box displays the Machine CoordSys. Confirm the CoordSys Manager dialog box with the Finish button. The Milling Part Data dialog box is displayed again. 8. Automatic Definition of the Stock and Target By default, the Stock and Target models are defined automatically. Once you have defined the Coordinate System, the Stock and Target buttons show that both Stock and Target models are chosen. Therefore, you can skip two following steps. Alternatively, if your default settings were changed in the Automatic CAM-Part definition page of the InventorCAM Settings, the buttons are not selected and you have to define the Stock and/or Target models manually. 9. Define the Stock model For each Milling project, you can define the Stock model, which is the workpiece that is placed on the machine before you start machining the CAM-Part. Click the Stock button in the Stock & Target model area of the Milling Part Data dialog box.
19 2. CAM-Part Definition The Model dialog box is displayed. This dialog box enables you to choose the mode of the Stock model definition. Stock model definition modes • Box – in this mode InventorCAM automatically determines the box surrounding the model. • Extruded Boundary – this mode enables you to define the 2D stock geometry with the chain of geometrical elements (lines, arcs, splines, edges, etc.). • 3D Model – this mode enables you to define the stock model via 3D model selection. • Cylinder – this mode enables you to define the stock model as a cylinder (or a tube) surrounding the selected solid model. • STL file – this mode enables you to define the stock model based on a STL file that exists in your system. When you choose this mode and click the Define button, the Choose STL dialog box is displayed. This dialog box enables you to choose the STL file for the stock definition. Choose the Box mode from the Defined by list. This dialog box enables you to select a solid body for the surrounding box calculation. Optionally, offsets from the model can be defined. In this exercise, define the stock model offsets as follows:
20 • For the X+, X-, Y+ and Y- offsets, set the values to 2; • For the Z+ offset, set the value to 0.25; • For the Z- offset, set the value to 5. Click on the solid body. It is highlighted. InventorCAM automatically generates the surrounding box. Confirm the Stock model definition by clicking the Finish button. The Milling Part Data dialog box is displayed. 10. Define the Target model InventorCAM enables you to define the Target model, which is the final shape of the CAM-Part after the machining. The Target model is used for the gouge checking in the SolidVerify simulation. Click the Target button in the Stock & Target model area of the Milling Part Data dialog box. The Target Model dialog box is displayed. This dialog box enables you to define a 3D model for the Target.
21 2. CAM-Part Definition Click the solid body. It is highlighted. Confirm the selection with the Finish button. The Milling Part Data dialog box is displayed. 11. Save the CAM-Part data Confirm the Milling Part Data dialog box by clicking the Save & Exit button. The Milling Part Data dialog box is closed, and the InventorCAM Manager is displayed. The defined CAM-Part is saved. At this stage, the definition of the CAM-Part is finished. The definition of Milling operations is covered in the following exercises using this CAM-Part.
22 The structure of the CAM-Part The CAM-Part includes a number of data files represented on the illustration that displays the data included in the CAM-Part named Milling. The Milling.prt file is located in the InventorCAM User directory. The Milling subdirectory contains all the data generated for the CAMPart. InventorCAM copies the original Autodesk Inventor model to the Milling subdirectory and creates an Autodesk Inventor assembly that has the same name as the CAM-Part (Milling.iam). There are two components in this assembly: DesignModel.ipt – a copy of the Autodesk Inventor model file. CAM.ipt – a file that contains InventorCAM Coordinate System data and geometry data. The InventorCAM CAM-Part uses the assembly environment of Autodesk Inventor. This enables you to create auxiliary geometries (e.g. sketches) without making changes in the original design model. You can also insert some additional components into the assembly file such as stock model, CNC-machine table, clamping and other tooling elements. The InventorCAM Manager is displayed. The definition of the CAM-Part is now complete. Milling.prt Milling.IAM CAM.IPT DesignModel.IPT Milling
23 2. CAM-Part Definition The InventorCAM Manager tree is the main interface feature of InventorCAM that displays the complete information about the CAM-Part. The InventorCAM Manager tree contains the following elements: • CAM-Part header This header displays the name of the current CAM-Part. By rightclicking it, you can display the menu to manage your CAM-Parts. The Machine subheader is located under the CAM-Part header. Double-click this subheader to review your machine configuration and parameters. The CoordSys Manager subheader is located under the CAM-Part header. Click this subheader to display the CoordSys Manager that enables you to manage your Coordinate Systems. InventorCAM Manager CAM-Part header Operations Tool header Machining Process header Geometries header Operations header Fixtures header }
24 The Stock and Target subheaders are located under the CAM-Part header. Double-click these subheaders to load the Stock Model/Target Model dialog boxes that enable you to change the definition of the Stock/Target models. The Settings subheader is also located under the CAM-Part header. Double-click this subheader to load the Part Settings dialog box that enables you to edit the settings defined for the current CAM-Part. • Tool header This header displays the name of the current Tool Library. Doubleclick its icon to display the Part Tool Table, which is the list of the tools that are available to use in the current CAM-Part. • Machining Process header This header displays the name of the current Machining Process table. • Geometries header This header displays all InventorCAM geometries that are not used in the operations. • Operations header This header shows you all InventorCAM operations defined for the current CAM-Part. 12. Close the CAM-Part Right-click the CAM-Part header in InventorCAM Manager and choose Close from the menu. The CAM-Part is closed.
InventorCAM 2.5D Operations 3
26 InventorCAM offers you the following 2.5D Milling operations: In InventorCAM, an operation is a single machining step. A workpiece is usually manufactured using several machining steps and technologies. For each of these steps you can define a separate operation. An operation can be very complex, but it always uses one tool, one major geometry and executes one machining type, e.g. Profile Milling or Drilling. You can edit any single machining operation, change the operation sequence and generate the GCode, combining and splitting the operation list of your CAM-Part. The Machining Geometry has to be defined for each operation. The Geometry prompts InventorCAM what and where you want to machine. • A Geometry for Profile, Pocket, Contour 3D, Slot and T-Slot operations, and Toolbox cycles consists of a number of chains. Chain geometries are defined by selecting the following entities: edges of models, 2D curves, 3D curves, circles, lines and splines. Each chain is composed of one or more entities and defines an open or closed contour. • A Geometry for Face Milling operations can be defined by selecting solid models, faces or chains of model elements. • A Geometry for Drilling and Thread Milling operations consists of one or more points (drilling centers) that can be defined by a number of methods directly on the solid model. • A Geometry for Drill Recognition and Pocket Recognition operations is determined automatically by SolidCAM Automatic Feature Recognition functionality. 2.5D Milling Operations Slot T-Slot Pocket Drilling Pocket Recognition Face Milling Thread Milling Contour 3D Profile Translated Surface ToolBox Cycles Drill Recognition
27 3. InventorCAM 2.5D Operations Face Milling Operation This operation enables you to machine large flat surfaces with face mill tools. Profile Operation You can mill on or along a contour. The profile geometry can be open or closed. In profile milling you can optionally use tool radius compensation to the right or to the left side of the geometry. InventorCAM offers two types of profiling: • Milling a single profile to the specified constant or variable depth in one step or in several user-defined down steps. • Concentric profiles to the specified constant or variable depth; this type of profiling generates several concentric profiles that start from the defined clear offset distance from the profile, and finish on the profile geometry, thus clearing the area around the profile to a constant depth. Pocket Operation In pocket milling, you have to remove material from the interior of a closed geometry. InventorCAM offers two types of pocketing: • When a profile geometry consists of one or more profiles and none of them are enclosed or intersect with one another, each is milled as a separate pocket without islands. • When a profile geometry consists of several profiles, any profile that is enclosed or intersects with another profile is treated as an island. You can define an unlimited number of islands within a single pocket.
28 Slot Operation This operation generates a tool path along the centerline to the right or to the left of one or more profiles. Two types of slots can be defined: The Slot with constant depth operation machines the slot in several steps until the final depth is reached. In Slot with variable depth, the depth profile is also defined by a 2D section. The slot can be pre-machined using rough and semi-finish cycles. The finish cut produces a tool path according to the specified scallop height on the floor of the slot. With available parameters for a right and left extension and side step, you can mill a slot wider than the tool diameter. T-Slot Operation This operation enables you to machine slots in vertical walls with a slot mill tool. Drilling Operation This operation enables you to perform drills and other canned drill cycles. InventorCAM supports the canned drill cycles provided by your particular CNC-machine such as threading, peck, ream, boring, etc. If your CNC-machine has no canned drill cycles of its own, they can be defined using the General Pre- and Post-processor program (GPPTool).
29 3. InventorCAM 2.5D Operations Drill Recognition This Operation carries out a highly efficient drill recognition and geometry creation with the functionality of the AFRMmodule (Automatic Feature Recognition and Machining). In this operation drilling on different levels can be carried out. The drilling levels are automatically recognized but may be edited by the user. Pocket Recognition This Operation recognizes automatically pocket features at the target model and creates the necessary machining. Contour 3D Operation This operation enables you to utilize the power of the 3D Engraving technology for the 3D contour machining. In this operation, InventorCAM enables you to prevent the gouging between the tool and the 3D contour. Thread Milling Operation This operation enables you to generate a helical tool path for the machining of internal and external threads with thread mills.
30 Exercise #2: Cover Machining In this exercise, you use the CAM-Part defined in Exercise #1. You have to define several 2.5D operations in order to machine the model external faces, pocket and holes in the corners. In the process of definition of operations, you have to define the machining geometry, the tool and several technological parameters. 1. Open the CAM-Part Click InventorCAM 2013, Open. In the browser window, choose Exercise1 – the CAM-Part prepared in the previous exercise. The CAM-Part is loaded.
31 3. InventorCAM 2.5D Operations 2. Add a Face Milling operation In InventorCAM Manager, right-click the Operations header and choose Face from the Add Milling Operation submenu. The Face Milling Operation dialog box is displayed. In this operation, the upper face is machined.
32 3. Define the Face Milling geometry Click the New button ( ) in the Geometry page. The Face Milling Geometry dialog box is displayed. The Base Geometry section enables you to define the face milling geometry using the following methods: • Model This option generates a rectangle located at the XY-plane and surrounding the Target model and selects it for the Face Milling geometry. The rectangle chain is displayed in the Chain List section. Face Milling geometry
33 3. InventorCAM 2.5D Operations • Faces This option enables you to define the Face Milling geometry by face selection. The New button and the related combo-box enable you either to define a new faces geometry with the Select Faces dialog box or to choose an already defined geometry from the list. When the model faces are selected, InventorCAM generates a number of chains surrounding the selected faces. These chains are displayed in the Chain List section. • Profile This option enables you to define the Face Milling geometry by a profile. The New button and the related combo-box enable you either to define a new profile geometry with the Geometry Edit dialog box or to choose an already defined geometry from the list. The defined chains are displayed in the Chain List section. Face Milling geometry Selected faces Face Milling geometry
34 In the Base Geometry section, use the default Model option for the Face Milling geometry definition. Click the Define button. The 3D Geometry dialog box is displayed. This dialog box enables you to define the 3D Model geometry by selecting the following types of model elements: • Solid – only solid objects are selected; • Surfaces – only surfaces only are selected; • Both – both surfaces and solids will be selected. The CAD selection button enables you to select the 3D geometry with the Autodesk Inventor tools. You can select an object by clicking on it. When an object is selected, its icon is displayed in the list in the bottom of the dialog box. To unselect the object, click it again or right-click its icon in the list of selected elements and choose Unselect from the menu. To remove selection from all objects in the list, click Unselect all. Click on the solid model to select it. The model is highlighted, and its icon appears in the list. Confirm the 3D Geometry dialog box by clicking the Finish button. The Face Milling Geometry dialog box is displayed again. The rectangle is generated surrounding the Target model at the XY-plane. Confirm the Face Milling Geometry dialog box by clicking the Finish button. The geometry is defined for the operation.
35 3. InventorCAM 2.5D Operations 4. Define the Tool Switch to the Tool page of the Face Milling Operation dialog box. Start the tool definition by clicking the Select button. The Part Tool Table is displayed. The Part Tool Table contains all tools available for use to machine a specific CAM-Part. The Part Tool Table is stored within the CAMPart. This dialog box enables you to manage the tools contained in the Part Tool Table.
36 Currently, the Part Tool Table is empty. Define a new tool suitable for face milling. Click the Add Milling Tool ( ) button to start the tool definition. A new pane containing available tools is displayed. This dialog box enables you to add a new tool to the tool library. In this operation, a face mill of Ø100 will be used. Face mill This tool type is used for machining of large flat surfaces. A tool of this type is defined with the parameters shown in the image. Outside Holder Length Cutting Length Arbor Diameter Diameter Tip Diameter Total Length Shoulder Length Angle
37 3. InventorCAM 2.5D Operations Choose the Face mill tool from the Tool type dialog box. Define the following parameters: • Set the Diameter to 100; • Set the Arbor diameter to 80. Choose the tool for operation by clicking the Select button. 5. Define the Face depth Switch to the Levels page of the Face Milling Operation dialog box. Click the Face depth button in the Milling levels area. This button enables you to define the Operation Lower level directly on the solid model. The depth is calculated automatically as a difference between Z-values of the Operation Upper and Lower levels.
38 The Pick Lower level dialog box is displayed. Select the model face as shown. The Lower level value (0) is determined and displayed in the Pick Lower level dialog box. Confirm this dialog box with the OK button. The Face depth value is displayed in the Milling levels area. The pink background of the edit box means that the parameter is associative to the model. Associativity enables the selected level to be synchronized with the solid model changes; InventorCAM automatically updates the CAM data when the model is modified. 6. Define the technological parameters Switch to the Technology page of the Face Milling Operation dialog box. In the Technology section, choose the One Pass option.
39 3. InventorCAM 2.5D Operations One Pass machining technology InventorCAM performs the face milling in one pass. The direction and the location of the pass are calculated automatically according to the face geometry, in order to generate an optimal tool movement with the tool covering the whole geometry. Selecting the One pass option automatically opens the One pass tab that enables you to define the machining parameters. The Extension section enables you to define the tool path extension over the face edges. The extension can be defined either by percentage of the tool diameter (the % of tool diameter option) or by value (the Value option). 7. Save and Calculate Click the Save & Calculate button. The Face Milling operation data is saved, and the tool path is calculated. Extension
40 8. Simulate Click the Simulate button in the Face Milling Operation dialog box. The Simulation control panel is displayed. Switch to the SolidVerify page and start the simulation with the button. The solid stock model defined in Exercise #1 is used in the SolidVerify simulation mode. During the machining simulation process, InventorCAM subtracts the tool movements (using solid Boolean operations) from the solid model of the stock. The remaining machined stock is a solid model that can be dynamically zoomed or rotated. It can also be compared to the target model in order to show the rest material. During the simulation, you can rotate , pan or zoom the model. Use these options to see the machining area in details. The Single step mode can be used to simulate the next tool movement by clicking the button or by using the space bar on your keyboard. Close the simulation with the button. The Face Milling Operation dialog box is displayed. Close this dialog box with the Exit button. 9. Add an operation Right-click the Face Milling operation entry in InventorCAM Manager and choose Profile from the Add Milling Operation submenu. The Profile Operation dialog box is displayed. In this operation, the external profile is machined.
41 3. InventorCAM 2.5D Operations 10. Define the Geometry The first step of definition of each operation is the Geometry selection. At this stage, you have to define the Geometry for the Profile operation using the solid model geometry. Click in the Geometry page of the Profile Operation dialog box. The Geometry Edit dialog box is displayed. This dialog box enables you to add and edit geometry chains. When this dialog box is displayed, you can select solid model entities for the Geometry definition.
42 Chain selection options You can define the geometry by selecting edges, sketch segments and points on the contour. The following options are available: Curve This option enables you to create a chain of existing curves and edges by selecting them one after the other. Associativity: InventorCAM keeps the associativity to any edge or sketch entity. Any change made to the model or sketch automatically updates the selected geometry. Curve + Close corners This option enables you to close the gaps between successive chain entities irrespective of the Gap Minimum and Gap Maximum values (defined in the Units Settings) by virtually extending the entities up to their intersection. Splines and arcs are extended by lines tangential to the arc/spline at its end point. First selected entity Next selected entity
43 3. InventorCAM 2.5D Operations Associativity: When the model used for the geometry definition is modified, InventorCAM enables you to synchronize the geometry with the updated model. During the synchronization InventorCAM determines gaps areas created using the Curve + Close Corners option and regenerates the extension of the chain elements so as to close the gaps. Loop This option enables you to select a loop by picking one of the model edges. 1. Pick an edge shared by two model faces. Two faces to which this edge belongs are determined, and their loops are highlighted. The first determined loop is considered to be the primary and is highlighted with yellow color. The second loop is considered to be the secondary and is highlighted with white color. 2. Choose one of the loops. Click on any other edge comprising the face. You are prompted to accept the chain that is now highlighted with yellow color. Accept the chain with the Yes button. A closed geometry chain is defined on this loop, and the secondary loop is rejected. Associativity: InventorCAM keeps the associativity to any edge or sketch entity. Any change made to the model or sketch automatically updates the selected geometry. Loop #1 Loop #2
44 Point to point This option enables you to connect specified points; the points are connected by a straight line. Associativity: InventorCAM does not keep the associativity to any selected point. InventorCAM saves the X-, Y- and Z-coordinates of the selected points. Any change made to the model or sketch does not update the selected geometry. You cannot select a point that is not located on an Autodesk Inventor entity (if you need to select such a point, add a planar surface under the model and select the points on that surface). The following rules apply to the virtual line selection using the Point to Point option: • When you select a virtual line between two edges, the line behaves as a spring. Whenever the model is changed and synchronized, the geometry is updated with the model. • When you select a sequence of several virtual lines, only the points connected to model edges or sketch elements are updated, but all other points stay fixed at the defined X-, Y- and Z-positions.